feed rate for thread milling op

[markfree27]

Is there a way you can add a reduced feed rate to a thread milling operation e.g. for arcing into the bore using a multiple tooth thread mill you would maybe want to arc in it at 50% of the feed rate you actually want to mill the helix path at....

[Kyle F]

I'm not 100% positive,.. but I wouldn't understand how you could get it to do that.

I've never had any issues with feed rate leading in on a thread mill either though,.. I tent to play it safe on the speeds/feeds while thread milling personally anyway.

 

These seem to be the only options on threadmill lead-in/out.

 

but actually,.. now that I'm thinking about it... technically you could draw wireframe in the geometry of your toolpath and you could 3d chain on that,... then for lead in/out you have a box for 'override feed rate' haha so I guess it's possible but IMO the juice ain't worth the squeeze.

[crazy^millman]

33 minutes ago, Kyle F said:

I'm not 100% positive,.. but I wouldn't understand how you could get it to do that.

I've never had any issues with feed rate leading in on a thread mill either though,.. I tent to play it safe on the speeds/feeds while thread milling personally anyway.

 

These seem to be the only options on threadmill lead-in/out.

 

but actually,.. now that I'm thinking about it... technically you could draw wireframe in the geometry of your toolpath and you could 3d chain on that,... then for lead in/out you have a box for 'override feed rate' haha so I guess it's possible but IMO the juice ain't worth the squeeze.

How we use to do in the V9 and previous days. draw a Helix and use 3D Contour. Back then we got Helix arcs without having to use the Arc3D Chook to get them.

[jpatry]

6 hours ago, markfree27 said:

Is there a way you can add a reduced feed rate to a thread milling operation e.g. for arcing into the bore using a multiple tooth thread mill you would maybe want to arc in it at 50% of the feed rate you actually want to mill the helix path at....

Yes, but not in the Threadmill toolpath.

You'd have to set up a Contour Ramp, with a pitch rate of your thread, then in the Lead In-Lead Out setting of contour you can set a feedrate override.

[crazy^millman]

9 hours ago, jpatry said:

Yes, but not in the Threadmill toolpath.

You'd have to set up a Contour Ramp, with a pitch rate of your thread, then in the Lead In-Lead Out setting of contour you can set a feedrate override.

Don,t forget to use Arc3D chook to reduce the NC Code. The best filter still gives this a fit.

[JoshC]

the best option i can think of to accomplish this is using the toolpath editor, create the path exactly the way you want it to be, then use toolpath editor to make that feedrate adjustment by right clicking on the toolpath and choosing toolpath editor and then making the change in the toolpath editor, that should be easy enough.

[crazy^millman]

5 hours ago, JoshC said:

the best option i can think of to accomplish this is using the toolpath editor, create the path exactly the way you want it to be, then use toolpath editor to make that feedrate adjustment by right clicking on the toolpath and choosing toolpath editor and then making the change in the toolpath editor, that should be easy enough.

Any changes to anything and all of that is lost. By doing with with an operations speeds and feeds will always stick and not be lost with a regeneration. Yes would still have to run the Arc3D chook since filter is tore up from the floor up doing a helix in a contour toolpath, but with tool path Editor a programmer runs the risk of losing those adjustment and having to remember them.

[cruzila]

This came up recently in a previous thread IIRC.

Better lead-in control in the software might be good but not sure what applications it really would make a difference in?  Step over control should accommodate any issues? There is a helix on entry option that would allow the tooth to follow the thread a little better on entry.

Edumacate me...........

[Kyle F]

20 hours ago, crazy^millman said:

How we use to do in the V9 and previous days. draw a Helix and use 3D Contour. Back then we got Helix arcs without having to use the Arc3D Chook to get them.

I'm going to have to take a peek into this arc3d chook,.. I am very unfamiliar (really only ever used findoverlap)

but a few of our machines are 20yr old 3axis' that have max memory of 1MB haha so I'm constantly using arc filters.

[Tim Johnson]

On 9/15/2023 at 8:43 AM, JoshC said:

the best option i can think of to accomplish this is using the toolpath editor, create the path exactly the way you want it to be, then use toolpath editor to make that feedrate adjustment by right clicking on the toolpath and choosing toolpath editor and then making the change in the toolpath editor, that should be easy enough.

 

19 hours ago, crazy^millman said:

Any changes to anything and all of that is lost. By doing with with an operations speeds and feeds will always stick and not be lost with a regeneration. Yes would still have to run the Arc3D chook since filter is tore up from the floor up doing a helix in a contour toolpath, but with tool path Editor a programmer runs the risk of losing those adjustment and having to remember them.

To save what you modified is add a Manual Entry under your tool path, copy your modified tool path into the Manual Entry then turn the Manual Entry off (ghost it out). If you have to regenerate the path your modification is still there to load it back in.

[markfree27]

Thanks everyone for the replies and help.  I tend to take it easy with threadmills myself however I do use the vardex software at times to get feeds and speeds for their threadmills dependant on material… they usually have the lead in feed like 50% of the actual cutting feed. For instance for like an NPT thread mill where there is a lot of teeth engaged in the cut.  However I do usually just run it conservatively anyways.  Was more just out of interest if I was missing something. Only been using mastercam for 8 months or so, previously used solidcam and that was similar to the contour op in mastercam in terms of the feed rate for linking could be controlled for every type of op including threadmilling. 
thanks again for the help really appreciate it!